Hi everyone,
I couldn’t find any advice online that matched my problem, so I’m here to share what I’ve learned trying to thread-mill a bunch of blind M6 holes in 6061 aluminum without access to air-blast. This is a worst-case scenario for chip buildup because they can’t fall out the bottom of the hole, and there isn’t much turbulence to force them out the top. It took me seven tries to find settings that work under these constraints, and most of those attempts required me to manually extract the threadmill from a chip-clogged bore using pliers. Hopefully I can save someone the headache of figuring out how to make this work.
The Bore:
The first challenge was creating a clean bore to start from. I’ve never drilled on my high-speed spindle, so I bored the initial hole with a 1/8in single flute. My bores were 1/2in deep and only 5.15mm in diameter, so it was surprisingly difficult to find speeds and feeds that didn’t result in massive chip welding and a broken endmill. The trick was scaling back to a low RPM to give chips more time to move between cuts. This will also provide more time for heat to conduct into the workpiece and cutter. Typically you want to avoid this, but cooler chips seem less likely to weld themselves to the walls of the bore when re-cut.
- 1/8in single-flute endmill
- 5.15mm bore diameter (~65% thread engagement)
- 13k RPM (10k worked fine too in my tests)
- ~425 ft/min
- 0.001 in/tooth (linear), actually ~0.00274 in/tooth due to the helix
- 0.02 in helix pitch
- climb milling
Endmill is cool to the touch immediately after this op, but heat may build up over many bores due to the low surface speed. I didn’t use a finishing pass since we’re already over-sizing the bore.
The Threadmill:
I’m using a cheap 60 deg “M6x1.0” (4.8 mm diameter) three-flute single point threadmill from AliExpress. I based my initial attempts on the speeds and feeds tables provided by harvey tools, but those toolpaths all caused my cutter to weld itself into the bottom of the bore. Most recommendations online suggest cutting the threads in multiple passes, but this will guarantee failure without proper chip evacuation. The initial passes will fill the bottom of the bore with chips that your threadmill will plunge into on the following passes. As with the boring operation, using a high RPM will cause massive chip welding. I eventually found a recipe that worked by taking the chipload recommendations from harvey tools and pairing them with low RPM and a single full-depth pass.
- 4.8 mm diameter 60 deg 3 flute single point threadmill (the diameter will be reported somewhere by the manufacturer; it’s the diameter that the points sweep in their rotation)
- 10k RPM
- ~495 ft/min
- 0.00018 in/tooth (linear), actually ~0.00084 in/tooth
- 1 mm thread pitch
- 1.31 mm pitch diameter offset (6.11 mm major thread diameter - 4.8 mm cutter diameter)
- 3 pitches (3 mm) of unthreaded space at the bottom of the bore to accumulate chips
- climb milling
- only one pass
The cut didn’t sound amazing at full depth, but it completes and actually produces a thread without destroying the workpiece. You’ll see that the threaded hole will be completely filled with chips after the cutter retracts. It seems like they mostly build up beneath the cutter as the cut progresses. My test thread was a bit loose, but you could dial this in with wear compensation or in-computer.
Hopefully this can get someone into the ballpark; I was beginning to think it wasn’t possible 
.